# Deep Hole Drilling: Use Depth-to-Diameter Ratio Before You Quote

Calculate drilling depth-to-diameter ratio, understand why tool reach, chip evacuation and coolant change with deeper holes, and review deep holes in CAD before CNC quoting.

This guide covers general CAD workflows. CADProps supports STEP, IGES, SolidWorks parts and ZIP assemblies, STL, OBJ, 3MF, static GLB/GLTF, and bounded 2D DWG/DXF preview and measurement. Validated conversions are downloadable. Partial assemblies carry warnings; properties cover loaded geometry only.

A hole can look trivial in CAD and still dominate machining risk. One of the fastest screening numbers is its **depth-to-diameter ratio**, often written as `L/D` or “×D.” A 6 mm diameter hole drilled 18 mm deep is 3×D. The same 6 mm hole drilled 120 mm deep is 20×D.

That ratio does not by itself say whether a hole is manufacturable, but it changes the drilling problem. Longer tools are less stiff, chips have farther to travel, coolant delivery becomes more important and runout or straightness errors become harder to control.

Tool suppliers reflect this directly in their product ranges. Kennametal, for example, offers purpose-built `20×D`, `30×D` and `40×D` deep-hole drills with internal coolant. One current 4 mm `40×D` product lists a maximum drilling depth of 160 mm. See Kennametal's [KenDrill Deep HPR 40×D example](https://www.kennametal.com/us/en/products/p.7080395.html).

## Calculate L/D before arguing about a “deep” hole

Use:

`depth-to-diameter ratio = drilled depth / hole diameter`

Examples:

| Diameter | Drilled depth | L/D | First impression |
|---:|---:|---:|---|
| 10 mm | 20 mm | 2×D | Ordinary depth for many workflows |
| 6 mm | 36 mm | 6×D | Tool reach/chip evacuation deserve attention |
| 5 mm | 100 mm | 20×D | Specialized deep-hole tooling/process may be appropriate |
| 3 mm | 90 mm | 30×D | Very slender drilling problem; process planning is critical |

The labels in the last column are deliberately qualitative. Material, tolerance, machine, coolant, entry/exit condition and tool family can change what is practical.

## Do not confuse hole depth with total feature length

CAD drawings and quoting systems can use “depth” differently. For a blind hole, distinguish:

- cylindrical full-diameter depth;
- drill-point depth;
- overall drilled depth;
- thread depth if the hole is tapped;
- counterbore or countersink depth.

If a drawing says `Ø6 DEEP 30`, verify what that callout means in the controlling standard and drawing convention. A supplier may need extra drill travel for the point even when the required full-diameter cylindrical portion is 30 mm.

For a through hole, workpiece thickness is not always the total tool travel either. Entry geometry, breakthrough and fixturing matter.

## Why L/D changes the process

### Tool stiffness

A longer drill is more flexible. Deflection can affect straightness, positional accuracy and hole quality. A short, stub-length drill and a 30×D drill of the same diameter should not be treated as equivalent tools.

### Chip evacuation

Chips generated near the bottom of a deep hole have to travel farther before leaving the cut. Packing, recutting or poor evacuation can damage the tool and surface.

### Coolant delivery

Deep-hole tools commonly use internal coolant because fluid needs to reach the cutting edge and help move chips out of the bore. The existence of 20×D, 30×D and 40×D internal-coolant product families is a useful reminder that deeper drilling is a process category, not merely “the same drill but longer.”

### Entry and exit conditions

Starting on an angled or interrupted surface can make guidance harder. Breaking through onto another surface can create burr or tool-loading problems. Tool suppliers often call out inclined-entry or inclined-exit suitability separately for exactly this reason.

## A deep hole is not automatically expensive if the design gives the process room

Depth matters, but so do tolerance and finish. A relatively deep clearance hole with generous positional tolerance can be easier than a shallower bore with tight diameter, straightness, surface finish and location requirements.

Before assuming a quote is high because of L/D, ask what the shop is controlling:

- diameter tolerance;
- position tolerance;
- straightness;
- surface finish;
- concentricity with another feature;
- blind-hole bottom condition;
- burr condition at breakthrough;
- material and heat treatment.

The expensive feature is often the **combination** of depth and precision.

## Review deep holes in the CAD model before sending RFQ

A useful manual review is:

1. confirm model units;
2. identify the small-diameter holes;
3. record diameter and actual drilling depth;
4. calculate L/D;
5. note whether each hole is blind or through;
6. check entry and exit surfaces;
7. record any counterbore, countersink or thread requirement separately;
8. add drawing tolerances and finish requirements to the same review.

CADProps can help with only part of this. The [STEP viewer](https://www.cadprops.com/tools/step-viewer/index.md) can inspect supported geometry, and the current feature analysis can classify **simple complete cylindrical through holes and flat-bottom blind holes in bounded cases**. It does not certify deep-hole machinability, tool selection, coolant strategy or a drilling cycle.

Use [STEP hole recognition](https://www.cadprops.com/guides/step-hole-recognition/index.md) as geometry evidence, not as an automated manufacturing plan.

## Do not turn a rule of thumb into a fake manufacturing limit

You will see rules such as “anything over 5×D is a deep hole” or recommendations to redesign above a certain ratio. They can be useful screening heuristics, but modern drill families span much larger ratios, and specialized gun drilling goes farther still.

The correct engineering conclusion is not that 20×D is impossible. It is that **a 20×D hole belongs in a different planning conversation than a 2×D hole**.

That conversation should happen before the part is released, especially if the hole is small, blind, angled, tightly toleranced or located where tool access is limited.

## Put the intent in the RFQ package

For a deep hole, do not send only nominal CAD geometry. Include the requirements the shop cannot infer safely:

- final diameter and tolerance;
- full-diameter depth / through condition;
- positional tolerance;
- surface finish if controlled;
- thread callout if applicable;
- material and heat treatment;
- deburr/breakthrough requirements;
- inspection requirement for depth or straightness.

The broader [STEP file for CNC quote checklist](https://www.cadprops.com/guides/prepare-step-file-for-cnc-quote/index.md) covers the rest of the RFQ package.

A depth-to-diameter ratio is valuable because it turns “that hole looks deep” into a measurable design-review signal. **Calculate it early, then use it to decide which holes deserve a real manufacturing discussion.**

## Related reading

- [Autodesk Fusion AutoTimeline: Why CAD Feature Recognition Matters Again](https://www.cadprops.com/guides/autodesk-fusion-autotimeline-feature-recognition/index.md)
- [CNC Internal Corner Radius: Design Pockets for Real End Mills](https://www.cadprops.com/guides/cnc-internal-corner-radius/index.md)
- [Minimum Wall Thickness for CNC Machining: No Single Safe Number](https://www.cadprops.com/guides/cnc-minimum-wall-thickness/index.md)
- [Prepare a STEP File for a CNC Quote: A Shop-Ready RFQ Checklist](https://www.cadprops.com/guides/prepare-step-file-for-cnc-quote/index.md)
- [STEP Hole Recognition: Detect Through and Blind Holes](https://www.cadprops.com/guides/step-hole-recognition/index.md)

Original article: https://www.cadprops.com/guides/deep-hole-drilling-depth-to-diameter-ratio/

HTML page: https://www.cadprops.com/guides/deep-hole-drilling-depth-to-diameter-ratio/